No announcement yet.

to climb or not to climb?

  • Filter
  • Time
  • Show
Clear All
new posts

  • to climb or not to climb?

    What do you think? What are your guidelines for climb milling or conventional milling.

    My ISCAR sales guy dropped off a trial tool with instructions for feed, speed and said, "climb mill whenever you can". I used the tool in a new CNC bedmill and wasn't very happy with the results. He said, "the ways and backlash" need adjusted. So, the machinery dealer sent a tech in for an inspection. We did a few tests and the tech pointed out that the problem was from "climbing" not slop in the machine.

    My complaint was poor surface finish around radius profiles.

    My machine is new with box ways in Y and dovetails in X. Ballscrews in both.

    So, the question is? What are your personal guidlines for when you can climb and when you should mill with conventional rotation?

    roughing? finishing?

    This is somewhat new to me as my prior experience has been with a worn out acme screw Bridgeport and you simply never climbed without a wreck.


  • #2
    Your Iscar rep is right you allways climb with indexable mills. If you are trying to run an indexable mill on a machine that is made similar to a Bridgeport you will have trouble.

    Indexable mills have to run very hard as compaired to regular end mills and small machines can have trouble providing the rigidity and horsepower nescessary to drive them correctly.

    Pass along a little more info about the machine, material and size of the tool. I can tell you from experience that salesmen blame someone else when they don't know how to fix a problem.

    [This message has been edited by C. Tate (edited 04-23-2002).]


    • #3
      Always climb....climb cutting is now refered to as "chip thinning"...

      It is funny that you bring up iscar...I just bought a 1.0" dia. 3-flute indexable mill from iscar about 2 months ago..

      I was cutting D2 tool steel and I first started to conventional worked, but my finish was I then changed my program to climb cut...My finish was absolutely depth of cut was .156, radial DOC was about .150 and my RPM's was 1300 with a feed rate of 24 in/min....It was beautiful....This was also ran DRY...

      What material are you cutting, and what grade of insert are you using...tool steel uses basically the same grade as stainless, which is a IC 328...if you are cutting 4140 or something very similar, then use grade IC 928..these grades are for Iscar only...



      • #4
        I have to agree with both of the above. Local reps usually don't know their ass from a hole in the ground with new products - it takes them a while to clue in. He may have given you incorrect feeds and speeds or the machine may not be up to it.

        Climb milling will always give better results in finish providing the machine has ball screws and the power to keep control of the workpiece. When you climb mill the bit takes maximum bite at the start of the cut. It starts out as a somewhat negative approach angle but exits as highly positive - resulting in a better finish. There is a tendency to fully eject the chip as well - conventional milling almost always brings them back around and the cutting edge will catch a portion of the old chip again before cutting the new chip.

        As Brent has stated he milled his D2 dry. With inserts, it is extremely important to either run dry or flood the crap out of it! Insufficent coolant (or uneven cooling with cold air) will cause failure of the inserts from thermal shock.


        • #5
          Thanks for the responses folks,

          My Machine is an ATrump B5EC Bed Mill. 5hp on the spindle and the overall machine weight is at 5000 lbs.

          The tool is a 1" indexable end mill with 3 inserts. The material is SAE1018 CRS. Spindle speed is 1800rpm, feed approx 30ipm and the DOC is .250" in Z.

          The work piece is 1" thick x 2" wide and I'm cutting a 2" dia round on the end which was previously saw cut square. The radial DOC varies as the tool rounds the square end of the bar. It enters at a tangent and exits tangent after making a 180degree arc.

          The chips were nicely ejected with a shiney silver color which then turned bluish when they settled in the pan. No coolant.

          The biggest complaint was that the work piece had a distinct line in the arc and the subsequent steps from the tools didn't line up. My thought was that the line was caused when the forces on the ball screw changed direction as the cutter crossed over the center of the arc. However, the line was not in the center of the arc but rather about 45degress off the center line. This also corresponds to the greatest amount of material to be removed. (the corner of the bar)

          Overall, I felt that the tool and machine performed well. The tool settled into the work nicely and the chips sprayed out a roostertail.

          Brent, from your note, I wonder if I'm taking too heavy of a cut. Even though D2 is much tougher than 1018....?

          Also, I'm not making a finishing pass.

          I have 2 different boxes of inserts. I've only tried 1 type...which I'm not sure the grade off hand and will need to run out to the shop to see. It was the first choice from the sales rep for the 1018 job, the other insert was his choice for an aluminum job.

          Thanks for the help,


          • #6
            May I ask a question? In above discussions what is DOC referring to?
            Lynn (Huntsville, AL)


            • #7
              DOC = Depth of Cut
              Mike L
              Amateur machinist, self-taught. I had a poor teacher, but I was a good student.


              • #8
                Ah so! Shucks, now it's obvious.
                thnx Mike
                Lynn (Huntsville, AL)


                • #9
                  You're gonna have to reduce your depth of cut.
                  Those salesman will promise you the world to make a sale.
                  Used to run an Ingersol slab mill with three 35 horsepower heads, and that mill couldn't take a 1/4 " finish cut.
                  Had to drop down to 1/32 or so for a blended precision like finish.
                  You're makin too much heat and either the part, or the cutter, or both are warping, or flexing making steps.
                  Coolant will help some.


                  • #10
                    Used to run an Ingersol bed miller, 8 inch dia. cutter, two inches d.o.c. 5 IPM. for a distance of between 4 to 12 feet. The spindle drive motor was 100 h.p. Machine table was 24 feet long and 6 feet wide. On it were two gargantuan magnetic/hydraulic clamps each wieghing approx. 20 tons, into which we could put a hunk of die steel (4150) up to 6 feet wide 2 feet thick and 20 feet long. If you do the math with die steel wieghing 501 lbs. per cubic foot that come to 60 Tons. That machine was the small one.

                    Paul G.
                    Paul G.


                    • #11
                      The step you are getting is from the angle that is built into the cutting edge of your insert. You will not be able to eliminate the step without a finish pass with a regular end mill. You can try a "square shoulder" mill that will not have the angle built into the insert, they are made so that they do not leave the steps you are talking about. Try decreasing the depth of cut on your current tool and the step will deminish some. I would decrease the chip load it sounds very high for your machine and the tool. Try 2200 rpm and 26 ipm that will give a chip load of .004 per flute at heavy radial DOC.

                      [This message has been edited by C. Tate (edited 04-25-2002).]


                      • #12
                        We had an 84, a 72, and a 66" Ingersol planer type mills. The 72" had a 24 foot table I think.

                        Usually used 8-10" shear clear cutters but 1/4" doc on a 10" carbide cutter and you're running in the red.

                        They were hosses. We machined coke oven doors and door jambs as well as frames and bases for cardboard box machines.

                        The 84" had four 35 hp heads. We made a ton of steel chips a shift on that one, using two heads.

                        That's when machinists had to work for a living. Got home looking like a coal miner from c.i. dust, way lube oil, and sweat.

                        Work your --- off for four hours setting up, and make chips for eight on some jobs.

                        Had three 18 ton cranes overhead busy all day loading machines.

                        Good old days? Old days anyway.
                        That was Koppers Company Machine Shop # 1.

                        Also had two 84" planers (Grey), four Devlieg Jig Mills, Two sellers and a fine King Boring Mill (84"), 84" Blanchard, and a load of other stuff.

                        That's gone now. Too many labor problems I guess.

                        They treat telephone poles and p. t. wood for decks now.



                        • #13
                          Ya the good old days. I'm glad I don't run that beast anymore. Still with the same company, just do a different job. Run two G & L 48 inch 4 axis cnc vtl's now. Cleaner and easier. But that is just the stuff that pays the bills, the real fun is out in the barn.

                          Paul G.
                          Paul G.


                          • #14
                            PAUL: I just have to know...What (or who) is in the barn? ;-) WALT


                            • #15
                              Sounds like if you want it to look real good you are going to have to run 2 passes. Non uniformity of cut is putting the pattern to it.

                              At least knock most of the corners off with the first cut.